5 axis?... Inclremental or Absolute perameters?

[Oscar R.]

So, most of the 5 axis jobs I program lately are low volume, quick turn around. That being said I don't always have the luxury of knowing where my part is going to be in the machine before starting my program.

In the past I could count on having all my gage lengths before starting, so I would program everything with absolute values.

I've been told that programing with incremental values will be needed now in order for me to be able to program my part ahead of time and move it later when I get the gage length from my set-up guy, then regen all my toopaths, and done.

 

Anyone out there use either method with this kind of situation with any success?

 

Thanks in advance for any help.

 

P.S. Table on table set up with preset tools.

[Guest CNC Apps Guy 1]

If by "5-Axis" you mean simultaneously cuttng in 5 Axes, those toolpaths are already in incremental so X Form Translate from... to... regen is fine.

 

If By "5-Axis" you mean positioning, a.k.a. 3+2, etc... then you will have to specify incremental on all aspects of your toolpaths to be able to just translate then regen. It's a little unnerving to some because as machinists we think absolute in terms of G90/G91. This is not the case n this particular situation. Absolute in MC mens the absolute position of the depth, top of stock, feed position, retract, clearance, etc... Incremental, just means the distance form the geometry you selected to where you want to be. Toolpaths still come out absolute (unless otherwise secified in a Misc. Real/Int.)

 

 

 

 

[Jaz]

I have always programmed almost everything with incremental values because it makes it easier for me to make changes later. That said, I don't know why it would make any difference which method you use while programming. It is the post that needs the gauge lengths, MasterCam doesn't really care as long as you are driving toolpaths to the tip of the tool. Unless you're doing things way different than anything I've ever seen.

[Oscar R.]

If by "5-Axis" you mean simultaneously cuttng in 5 Axes, those toolpaths are already in incremental so X Form Translate from... to... regen is fine.

 

If By "5-Axis" you mean positioning, a.k.a. 3+2, etc... then you will have to specify incremental on all aspects of your toolpaths to be able to just translate then regen. It's a little unnerving to some because as machinists we think absolute in terms of G90/G91. This is not the case n this particular situation. Absolute in MC mens the absolute position of the depth, top of stock, feed position, retract, clearance, etc... Incremental, just means the distance form the geometry you selected to where you want to be. Toolpaths still come out absolute (unless otherwise secified in a Misc. Real/Int.)

 

Apps Guy, first off thanks for the reply.

The way you've just laid it out is the way I've been trainned and work 5 aixs.

I could of sworn I've done this in the past with no problem. Both simultanious 5 axis and 3+2. I do understand the difference between the absolute and incrementals in MasterCam vs. machine absolute and incremental.

Yet for some reason with the programs I've been working on lately I'm having issues with some of my toolpaths following my geometry after x form translate(all values in absolute). I try to always program to center of rotation using plane selection in WCS as needed for 3+2. So my geometry realy only gets moved in Top Z from center of rotation, when I get my gage length.

Tools for simultanious are set from center of the tool and tip for 3+2.

I've also tried choosing the same geometry with incremental values and get the same results.

 

I know it's something I'm missing, just not sure where.

Just getting a little steamed besause as things are now, I have to re-choose most of my values once i finally get my gage lengths in order to get a good program. It's like doing everything twice, big time burner.

 

I'll go over a few more toolpaths and try to see if I catch anything. Then report back mid morning.

 

Thanks agian for the help.

[Oscar R.]

I have always programmed almost everything with incremental values because it makes it easier for me to make changes later. That said, I don't know why it would make any difference which method you use while programming. It is the post that needs the gauge lengths, MasterCam doesn't really care as long as you are driving toolpaths to the tip of the tool. Unless you're doing things way different than anything I've ever seen.

 

Jaz

I think it's slowly starting to come back to me. Like I mentioned in Apps Guy's reply, I'm almost sure it's something I'm missing.

Moslty I'm looking to verify that it can be done either way and still get a good program. Also which method is most commonly used successfully in this type of situation.

I think App Guy's break down realy sums it up. And your post helps verify it.

 

Thanks for the input.

[Bruce Caulley]

I might be in the minority, but I've always used absolute. Having said that all but a few of the 5-axis machines I have programmed for used either TCP or dynamic work offsets. For the ones that didn't I measured where the 4/5 axis intersection was and then used that as my nominal origin in MC. Outputting a different work coordinate for each view then allowed me to tweak where necessary, but if a part was no tighter than 0.1mm tolerance it was usually good enough.

 

What machine may I ask?

 

Bruce

[Teh Bear without Brains kinda idiot]

I always use incrimental cause some of my machines have and some have not dynamic work offsets.

This way I am able to program the part so that I can do it on any our 5 axis machine

 

BR

[Tinhman]

absolute for 3 , 4 axis and Incremental for 5 axis. It is just easier for me to move thing around.

[Oscar R.]

I might be in the minority, but I've always used absolute. Having said that all but a few of the 5-axis machines I have programmed for used either TCP or dynamic work offsets. For the ones that didn't I measured where the 4/5 axis intersection was and then used that as my nominal origin in MC. Outputting a different work coordinate for each view then allowed me to tweak where necessary, but if a part was no tighter than 0.1mm tolerance it was usually good enough.

 

What machine may I ask?

 

Bruce

 

Bruce, it sounds like your non-dynamic work offset set-up is what I'm used to working with.

I used to use that method on old Haas HS-1 horizontals with custom trunnion style set-ups on them. Currently I working on an Okuma VMC with a Kuma 0. to -90. rotary attachment(somewhat limited on this one). But in about a week we're getting a brand spankn' new Matsuura MX-520 so I want to knock the webs out of all my 5 axis stratigies before then.

[Oscar R.]

Been working on this on a bit this morning and I seem to have seen a pattern on some of my toolpaths.

On all of the tolpaths that let me choose my linking perameters in incremental everything works fine when I X Form then rengen. But on the HS toolpaths like OptiRough and Core Roughing that only let me use the steep/shallow perameters to choose a Z depth, my toolpaths won't follow when I X Form move my geo and regen. I have to go back into my perameters on those toolpaths and adjust my Z depths one by one.

Not fun when I have over 80 toolpaths to keep track of.

[Guest CNC Apps Guy 1]

...But on the HS toolpaths like OptiRough and Core Roughing that only let me use the steep/shallow perameters to choose a Z depth, my toolpaths won't follow when I X Form move my geo and regen. I have to go back into my perameters on those toolpaths and adjust my Z depths one by one.

Bingo... IIRC, the HST Toolpaths on the Steep/SHallow parameters are absolute. Sorry to say, you'll have to reselect the depths on the steep/shallow settings every toolpath unfortunately.

 

CNC, can we get an enhancement please?

[Oscar R.]

Yup, that's it.

I wish we had an option with these toolpaths. I really like the HS toolpaths and I I've started to use them pretty often. Just a bummer they won't be as productive in my 5 axis programs unless something changes either on the MC side or the way set-ups are done here.